Eliminating twisting from sweep around a helix

[spopa2]

Hello,

 

I am having trouble modeling a multi-layered solenoid in solidworks. The issue arises when I sweep a sketch around a 3D curve that describes my helix. Although the sweep is done as "follow path" the shape is produced correctly for the first turn after which it starts sloping instead of staying horizontal to the top plane like I want it to. Please let me know if you have any ideas on how to fix this. I cannot attach my file here but you can find it at this link :http://www.eng-tips.com/viewthread.cfm?qid=298129&page=1

 

Cheers,

 

Sorin

[SLW210]

Are you using Solidworks?

[spopa2]

yes. Also, this sweep of multiple circles that i am trying to do works perfectly if my cross section is an ellipse. The problem arrises when I try to use a rectangle with semicircle on the ends.

[JD Mather]

Attach your *.sldprt here (roll up the feature tree and zip before attaching).

[SLW210]

I have moved this to the Solidworks section for you.

[shift1313]

The first thing to do is create a plane at the end of your 3d path. This plane needs to be normal to the path so you keep your profile the same as it is swept. The next thing is to deal with the options within sweep. There are a few options, one of which is Twist Along path with Normal Constant. Give that a shot.

 

I talk about part of this here:

 

http://www.solidworkslessons.info/#!__features-sweep

[spopa2]

Thank you for the reply. I have tried what you said but it will not let me "twist along path with normal path, the only option that works is "follow path" and "twist along path". twist along path does exactly what I dont what it to do. I want the profile to not change its angle as it twists up the helix, I want it to stay parallel to the top plane as it rises and for some reason follow path does not let it do that.

 

What is weird is that using the same methods but making a solenoid with a elliptical cross section does not produce this problem.

 

JD, I cannot attach the file as it is larger then 250k even when rolled back and zipped. Please follow the link http://files.engineering.com/getfile.aspx?folder=cd6bb75d-576d-496e-88dc-16aa538e17b4&file=solenoid_multi_connected.SLDPRT to where you can download the file.

 

Thanks again for the help!

[bhamze]

Have you tried to create each sweep individually? I gave it a shot, see attached photo. The model on the left was created with four individual sweeps, your model is on the right. Is this what your trying to accomplish?

 

[spopa2]

Thanks bhamze, that looks perfect.

 

I need to be able to modify the parameters for this, like the number for turns, the thickness of the wire and the number of wires. I am planning to do this with drive works express. Do you think this will be more easily done with your method or my method?

 

Also, I need to be able to alternate the hight of each wire, as show in the sketch i attached. When they were all one sweep this was all just done by patterning a sketch. How will this be achieved with individual sweeps?

 

Should each sweep be a different part, and then have them mated? Would this make more sense if i plan on automating the process with driveworksxpress?

 

Thanks again!

[bhamze]

I don't use Driveworks professionally, my only experience is what I gathered when learning the application. From what I can remember its similar to design tables. So I think either a design table or Driveworks will work in your case. Both our methods are the same, the only difference is the amount of sweeps. I'm not certain in what your trying to accomplish but I think all the parameters you mentioned can be modified easily with minimal effort. The use of equations or in-context modeling may be the solution. Are you familiar with these methods? What version of SW are you using?

[spopa2]

I'm using sw standard 2010. Im not familiar with in context modeling or equations. I have just begun looking into driveworksxpress.

 

I need to be able to have a way of easily imputing some parameters, like wire thickness, number of turns, number of layers, etc. And have models made based on these parameters quickly and with minimal manual input. Do you think equations/in context modeling or driveworks would be more suitable?

 

Also, can you upload the part file that you made with the individual sweep? Thanks again!

[bhamze]

The use of equations and/or in-context modeling are ways of linking geometry, allowing multiply changes with a single edit. From there you can create a design table that will control the features/dimensions you want to edit. Or if you prefer, use driveworks instead. Personally, I use design tables. When creating a design table you have the option of creating a custom view allowing only the fields you want visible. Check out link below. The video covers design tables,equations and custom views. I hope it helps. Regarding the file...it was created with SW2011. If your using 2010 you will not be able to open it.

 

 

 

http://www.solidworkslessons.info/#!__design-tables

[bhamze]

I had some time this morning so I gave you model another shot. The good news is that I was able to create the sweep as one feature. Whats strange is that I could only accomplish this using surface modeling. See attached pictures. Both are sweeps and both share the same input selections. Pay close attention to the path alignment type. In this field select direction vector and use the top plane as your reference. As you will see, the surface sweep gave you what your looking for. I'm not sure why the solid sweep gave different results. Maybe others can give it try, it may be a bug in my version of SW.

 

[shift1313]

spopa, even in drive works you need to plan out your sketches ahead of time and make use of linked dimensions, relations and equations to make this work. Are you looking to actually have someone input values, have the cad model made and then save it? With some of this functionality if you are truly trying to limit the users interaction(interference) you will need a lot more work on the front end.

 

When using driveworks you will create new files. When trying to use design tables you will create new configurations(or over-write the current one) and Save As Copy.

 

I would concentrate on setting up your model and modifying your values that you want to make sure your model updates. Driveworks will not simply allow you to change things if they arent properly defined.

 

If you can come up with a list of parameters you need to change maybe we can get you started on the right path. The setup for this is very very important.

[spopa2]

@bhamze: Thank you for all these attempts. The surface sweep is exactly what I am looking for, however I need the model to be a solid wire as it is going to be inputed into a magnetic field simulator. If we can not figure how to get the solid sweep to work is there a way to "fill in" the closed surfaces, thereby creating a solid model? Also, I just got sw 2011, so can you please upload your files, thanks.

 

@shift1313: I do not need to limit the users functionality, I will be the only one creating models. I just need to be able to input these parameters:

 

diameter of wire

number of turns

number of layers (number of wires side by side in the cross section)

 

I would also like to be able to change the cross section of the solenoid itself (as seen looking down on the top plane) from this "race track" shape, shown in the models above, to an ellipse or circle. I was planning on having each different cross section have its own driveworks file, however if I can have driveworks change this shape also then that would be ideal so I dont have to switch between driveworks models.

 

As of now I am in the process of going through some driveworks tutorials. Once I understand how to use it I will being thinking of rules and relations for my model.

 

If you can help me at all with the setup or give any more guidance it will be greatly appreciated.

 

Thanks again to all of you for you help!

[bhamze]

Here is the file. This was done rather quickly so it might be buggy. Right click on any equation to make dimension changes. Sweep 6 and sketch 13 lose their relations when making multiply/large dimension changes. I recommend you edit one equation at a time with small dimension values to avoid error.Make a copy of the model just in case . This will help you get a better understanding of linked values and equations. There are different approaches to accomplish what you need, this is only one example, Hope it helps.

 

http://www.4shared.com/file/zaaV8Hyw/solenoid_multi_connected.html

[spopa2]

Thank you bhamze for the file. It works pretty well. I am having an issue that I cant seem to solve:

 

I needed to change sketch 13, because I needed the wires in a different configuration. I used the sketch pattern in the y direction and then used "instances to skip" to get rid of the sketches I didnt need. My problem is that now the "number of layers" doesnt work because I cant figure out a way to use equations to drive the "instances to skip". Is there a way to do this?

 

Would it be easier to use a linear pattern for features and extrude each cylinder one at a time? Can this be equation driven in the way that I want?

 

Cheers

Edited May 9, 2011 by spopa2
wrong picture

[spopa2]

I actually managed to solve this problem by using two seperate linear patterns in the sketch and linking them with equations

[bhamze]

Im glad you got it sorted. Did you figure how to make your part solid?

[spopa2]

As of now I capped off the ends with a planer surface and then knitted each loop individally. This worked, however I am not sure how easily it will be automated through driveworks. If you dont think this will work I would really appreciate any suggestions you have.

 

Here is the link to the updated model if you want to check it out: http://files.engineering.com/getfile.aspx?folder=dc9d950c-fd11-4cee-a099-49b0181758e2&file=solenoid.SLDPRT

 

 

Cheers